|
[Sponsors] |
February 17, 2016, 00:04 |
I can't break FLUENT
|
#1 |
Member
Mike Tree
Join Date: Feb 2016
Location: Charlotte, NC
Posts: 37
Rep Power: 10 |
I cannot seem to force FLUENT to diverge. I realize this is a bit counter-intuitive, so let me explain.
I have a pipe flow for which I have specified a mass flow inlet boundary condition at one end and wall boundary conditions everywhere else, including what would normally be the pipe outflow. Running a steady pressure-based solver with coupled pressure-velocity coupling with least squares cell based, second order, and second order upwind for gradient, pressure, and momentum spatial discretizations, respectively, results in a CONVERGED SOLUTION! Of course, a converged solution doesn't guarantee a physically accurate solution. I explored the solution with some monitors which verified that my mass flow inlet boundary condition is as defined, the mass of the entire fluid volume is steady, and the spatially mean velocity magnitude of the fluid volume is steady as well. Plotting the velocity vectors shows zero velocity at the far wall (where the pipe outlet should normally be). Now, no one in their right mind would accept the solution I receive because it makes no sense. I am simply confused that FLUENT gives a solution at all. What am I not understanding about FLUENT'S continuity convergence? Shouldn't my fluid volume mass grow continually and prevent continuity convergence? Ultimately, I ran this simulation as a misguided effort to initialize a 2-way FSI case with FLUENT and ANSYS Mechanical via system coupling, but now my very understanding of fluid dynamics is crumbling. Any help will be appreciated. |
|
February 17, 2016, 04:00 |
|
#2 |
Senior Member
Join Date: Nov 2013
Posts: 1,965
Rep Power: 26 |
Interesting situation... What does your mass flux report say? I hope there the net mass flux is not close to zero, but (almost) equal to your inflow, but it is good to check.
And what do you call "converged solution"? The standard fluent settings for continuity residual < 0.001? In my opinion, for simple problems this number should be much smaller. |
|
February 17, 2016, 09:42 |
|
#3 |
Senior Member
Lucky
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 5,665
Rep Power: 65 |
One thing to note is that the mass-flow inlet does not enforce a uniform mass flux so it's possible to have some outflow (which may be doing some funny things to save the simulation).
Try using a velocity inlet instead of a mass-flow inlet to see if you can get the velocity inlet to diverge. |
|
February 17, 2016, 10:00 |
|
#4 | |
Member
Mike Tree
Join Date: Feb 2016
Location: Charlotte, NC
Posts: 37
Rep Power: 10 |
Quote:
My convergence criteria are set at absolute residuals <1e-07 for continuity and all three velocity directions. For reference, my total mesh volume is 2.206e-05 m3 and my fluid density is 1060 kg/m3, so the total mesh mass should be around 0.0234 kg. |
||
February 17, 2016, 10:16 |
|
#5 | |
Member
Mike Tree
Join Date: Feb 2016
Location: Charlotte, NC
Posts: 37
Rep Power: 10 |
Quote:
Mass Flow Rate (kg/s) -------------------------------- -------------------- inlet_vel 0.00099999993 interior-fluid -0.0029626614 outlet_wall -0 wall -0 ---------------- -------------------- Net 0.00099999993 |
||
February 17, 2016, 10:47 |
|
#6 |
Senior Member
Lucky
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 5,665
Rep Power: 65 |
I am concerned that your simulation actually calculated and didn't throw some type of floating point error or divergence error or divergence in amg solver error
However, I am not surprised that continuity residual criteria is met because of the way the continuity residual is calculated. The continuity residual is normalized by the worst residual in the first 5 iterations, and if the worst residual is very bad then the continuity residual can decrease, slightly better than very bad is still better. Dividing a large number by a very very large number results in a small number. I would focus on the detailed velocity field and figuring out what doesn't make sense and I wouldn't give any attention to the residual. |
|
February 17, 2016, 10:58 |
|
#7 | |
Member
Mike Tree
Join Date: Feb 2016
Location: Charlotte, NC
Posts: 37
Rep Power: 10 |
Quote:
|
||
Thread Tools | Search this Thread |
Display Modes | |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
Two questions on Fluent UDF | Steven | Fluent UDF and Scheme Programming | 7 | March 23, 2018 03:22 |
heat transfer with RANS wall function, over a flat plate (validation with fluent) | bruce | OpenFOAM Running, Solving & CFD | 6 | January 20, 2017 06:22 |
Fluent crash on writing data file after thousand iterations | Chuck87 | FLUENT | 0 | September 2, 2015 16:17 |
Fluent 12.0 is worst then Fluent 6.2 | herntan | FLUENT | 5 | December 14, 2009 02:57 |
Problems in lauching FLUENT | Lourival | FLUENT | 3 | January 16, 2008 16:48 |